An exclusive raffle opportunity for active members like you! Complete your profile, answer questions and get your first accepted badge to enter the raffle.
Hi experts,
Â
I was wondering if I could extract the volume of single tetrahedral element in the mesh using udf in acusolve. Do you think it is possible? I have a non-uniform unstructured tetrahedral mesh.
Thanks and regards,
Prabin.
I'm thinking the simplest (though not necessarily simple) approach is through this function call:udfGetOeiData() - where one of the fields is volume:https://help.altair.com/hwcfdsolvers/acusolve/topics/acusolve/udfgetoeidata_acusolve_udf.htm
This depends on having an ELEMENT_OUTPUT command in the input file like this:
ELEMENT_OUTPUT( "sample" ) { element_set = "flow" type = subset elements = { 32 ; } integrated_output_frequency = 1 integrated_output_time_interval = 60.0 num_user_output = 0 }
https://help.altair.com/hwcfdsolvers/acusolve/topics/acusolve/element_output_acusolve_com_ref.htm
The element number 32 has to exist in the element set "flow" defined elsewhere.
You'll need to pull your desired element number from the existing element set definition - to use in that ELEMENT_OUTPUT command.
I'm thinking the simplest (though not necessarily simple) approach is through this function call:udfGetOeiData() - where one of the fields is volume:https://help.altair.com/hwcfdsolvers/acusolve/topics/acusolve/udfgetoeidata_acusolve_udf.htm This depends on having an ELEMENT_OUTPUT command in the input file like this: ELEMENT_OUTPUT( "sample" ) { element_set = "flow" type = subset elements = { 32 ; } integrated_output_frequency = 1 integrated_output_time_interval = 60.0 num_user_output = 0 } https://help.altair.com/hwcfdsolvers/acusolve/topics/acusolve/element_output_acusolve_com_ref.htm The element number 32 has to exist in the element set "flow" defined elsewhere. You'll need to pull your desired element number from the existing element set definition - to use in that ELEMENT_OUTPUT command. Â
Do you know how can I calculate volume of each element in the mesh using acuReport? I found the following link:
https://help.altair.com/hwcfdsolvers/acusolve/topics/acusolve/elmvolume.htm
Do you know how can I calculate volume of each element in the mesh using acuReport? I found the following link: https://help.altair.com/hwcfdsolvers/acusolve/topics/acusolve/elmvolume.htm
What are you wanting to do with the element volume? What's the end goal with that information?
I have a domain of fluid where a particular region is solid. The solid region is random in its shape. However, I have identification (based on the element) that the region is solid. I will add the volume of all the elements to calculate the volume of that solid region.Â
This is simple representation of flow over cylinder. I basically want to calculate the volume of solid cylinder. It is simple for simple solid. As I move on, there will be more complex structures whose volume I need to calculate.Â
So, to help out with this, I am thinking of summing the volume of each element within this region. This will ultimately be used in the optimization of fluid flow.
I have a domain of fluid where a particular region is solid. The solid region is random in its shape. However, I have identification (based on the element) that the region is solid. I will add the volume of all the elements to calculate the volume of that solid region. This is simple representation of flow over cylinder. I basically want to calculate the volume of solid cylinder. It is simple for simple solid. As I move on, there will be more complex structures whose volume I need to calculate. So, to help out with this, I am thinking of summing the volume of each element within this region. This will ultimately be used in the optimization of fluid flow.
Are you doing topology optimization - as in these tutorials?https://help.altair.com/hwcfdsolvers/acusolve/topics/tutorials/acu/acu_7200_intro_sl_r.htm
https://help.altair.com/hwcfdsolvers/acusolve/topics/tutorials/acu/acu_7201_intro_sl_r.htm
So it's only during the simulation that the elements are determined to be either fluid or solid? Are you somehow adding a marker to call it 'solid'? If you're defining the geometry volumes as either fluid or solid and they don't change through the simulation, the ELEMENT_OUTPUT I mentioned before gives you volume as one of the output quantities.
(I guess I'm confused when you say 'I have a domain of fluid where a particular region is solid' - I would generally think a volume is either fluid or solid, not both.)
Are you doing topology optimization - as in these tutorials?https://help.altair.com/hwcfdsolvers/acusolve/topics/tutorials/acu/acu_7200_intro_sl_r.htm https://help.altair.com/hwcfdsolvers/acusolve/topics/tutorials/acu/acu_7201_intro_sl_r.htm So it's only during the simulation that the elements are determined to be either fluid or solid? Are you somehow adding a marker to call it 'solid'? If you're defining the geometry volumes as either fluid or solid and they don't change through the simulation, the ELEMENT_OUTPUT I mentioned before gives you volume as one of the output quantities. (I guess I'm confused when you say 'I have a domain of fluid where a particular region is solid' - I would generally think a volume is either fluid or solid, not both.)
I am not doing density-based TO. So, I could not use the built-in TO tools. Yes, I have a marker in each element for solid.
I could not use the method you explained earlier because I don't have exact solid volume set. My volume changes from fluid to solid (or vice versa) throughout the optimization process.
Do you know how I can use acuReport?
I am not doing density-based TO. So, I could not use the built-in TO tools. Yes, I have a marker in each element for solid. I could not use the method you explained earlier because I don't have exact solid volume set. My volume changes from fluid to solid (or vice versa) throughout the optimization process. Do you know how I can use acuReport?
I am not familiar with acuReport usage.
Have you tried using udfGetElmWDetJ in the user function?https://help.altair.com/hwcfdsolvers/acusolve/topics/acusolve/udfgetelmwdetj_acusolve_udf.htm
Looks like this is accessible from Body Force, Material Model, or Component Model user functions.
I am not familiar with acuReport usage. Have you tried using udfGetElmWDetJ in the user function?https://help.altair.com/hwcfdsolvers/acusolve/topics/acusolve/udfgetelmwdetj_acusolve_udf.htm Looks like this is accessible from Body Force, Material Model, or Component Model user functions.
I have been able to get the volume of single element (both in serial and parallel mode with 8 cores.) I used the code as mentioned in the above link. The following code works very well both in series and parallel. I found that wDetJ is 1/8 th of volume of single element. To find the volume of an element, I needed to multiply by 8 (most probably there are 8 gauss points).
Real* wghtDetJac ; Real wDetJ ; Integer elem ; ... wghtDetJac = udfGetElmWDetJ( udfHd ) ; for ( elem = 0 ; elem < nItems ; elem++ ) { wDetJ = wghtDetJac[elem] ; ... }
I have a simple geometry as below. It is 1m x 1m x 1m with (10 x 10 x 1) elements:-Â
Now, the issue I am having is that I have marker (0-fluid; 1-solid) for each element in the domain above. I want to run a code to calculate the volume of only fluid (i.e marker with 0). I wrote a code that does this. It works very well in series (only 1 core). But, I found when I try to run the same code in parallel (multi cores with 8 cores), wDetJ is correct. But, the total volume (vol) corresponding to 0 marker is not correct in parallel mode--it is correct only in series mode. Would you please help me figure out how to evaluate the volume for the 0 marker only in parallel mode? I figured out that UDF is called several times even in each timestep due to parallelization. The code I ran is:
